Dimmension values incorrect on drawing.

[Anonymous]

I'm using Inventor 2013.  I created an assembly where I did a lot of top down modeling (meaning components in the assembly were created in the assembly.  All but a handful of the components are adaptive to other components).  When I went to make my drawings for having the components made, I started noticing that some of the dimension values were wrong.  I could go into the model and verify the features, but when dimensioning on the drawing it would not match.  Furthermore, this didn't occur on every dimmension on the drawing.  Not even half of them were incorrect, but it only takes one to really mess up a part.

I've attached a screen shot of what I'm seeing.  The 15.2 and 5 dimmension are correct, but obviously those don't add up to 31.37.  I know I can manually override this dimmension, but only if I know to do it.  I tried to do a drawing of another part in the same assembly and eventually found a similar problem. 

Finally, I created a step file of the 1st part (to strip away the adaptivity) and when I created the drawing again, the problem went away.

My question is, is there something I did in the assembly / creation process that would have caused this? 

[JDMather]

Why post an xls for an image?

There is a lot in that image that isn't part of the problem description.

Tip - go to Start and in the Search box type Snip and select the Snipping tool to snip screen shots.

Save and attach *.png here.

On your problem

is it set to True Dimension or Projected Dimension (right click)?

[pcrawley · Accepted solution]

Right-click the view and select "General Dimension Type" > "Projected" (I suspect you have it set to "True").

If you look at the dimension text and the arrow heads, you'll see they are "squashed".  This is a good indication that you are working with true dimensions.

In case you are wondering, the difference is obvious when you understand it:  Looking down on a 45 degree cut on a piece of box-section, you see a line at 45 degrees.  When you look at the end view of the same shape, you see a nice rectangle.  A Projected dimension on the end view will report the dimensions of the box-section.  A True dimension will report the actual cut length of the miter face (the hypotenuse).  

(Probably not the best explanation, but hopefully it make sense.)

[Anonymous · Accepted solution]

I think your explanation makes perfect sense.  I've used Inventor for a couple of years, but don't consider myself proficient at it by any means.  I had never noticed that before on any of the previous versions, and it doesn't make a lot of sense to me why that would be the default setting (I was just using a standard default template for the drawing). 

Thank you so much for the tip.

[pcrawley]

No problem - although JD deserves the credit as he mentions the issue on the last line of his reply.  I didn't see his response until after posting mine.  Maybe I should start reading these posts on the website.

You need to watch out for this type of dimension as they can sneak up on you.  If view of a model is not orthographic to it's origin planes, then "True" dimensions will be the default.  (It does make sense when you think about it - it's how dimensions work on isometric views.)  

With the default behaviour of 2014 now NOT grounding the first component in an assembly, it is very easy to place a component that's off-axis by a fraction of a degree.  Subsequent drawings will therefore default to true dimensions and you may not notice because the degree of distortion of the text will be minimal, but the measured dimensions could be costly!  It would be useful if there was a checking tool that highlighted all True dimensions on a drawing.  Maybe next year.